김경종
320 lines
27 KiB
Markdown
320 lines
27 KiB
Markdown
<!-- source-page: 961 -->
|
||
|
||
Repeat the data line for three-dimensional cases to specify the crack front and virtual crack extension vector for each node (or cluster of focused nodes) along the crack line.
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front: Specify crack extension direction using: q vectors
|
||
|
||
# Defining surface normals
|
||
|
||
In a case where the crack front intersects the external surface of a three-dimensional solid, where there is a surface of material discontinuity in the model, or where the crack is in a curved shell, the virtual crack extension direction, , must lie in the plane of the surface for accurate contour integral evaluation. Surface normals should be specified at all nodes that lie on such surfaces within the contours requested for this purpose (these nodes are printed out under the “Contour Integral” information in the data file). For shell element models the normals can be specified with the nodal coordinates if the normals calculated by Abaqus/Standard are not adequate. For solid element models the normals can be specified either directly (see “Normal definitions at nodes,” Section 2.1.4, and “A plate with a part-through crack: elastic line spring modeling,” Section 1.4.1 of the Abaqus Example Problems Guide) or using the nodal coordinates (the fourth–sixth coordinates). If surface normals are not specified for the nodes on the crack surfaces and the external surfaces at the ends of a crack line, Abaqus/Standard will calculate the normals automatically for these nodes to correct any inadequate virtual crack extension directions, .
|
||
|
||
# Defining the data required for a contour integral with XFEM
|
||
|
||
If you are using XFEM to evaluate the contour integral, both the crack front and the virtual crack extension direction are determined by Abaqus/Standard.
|
||
|
||
# Symmetry with the conventional finite element method
|
||
|
||
If the crack is defined on a symmetry plane, only half the structure needs to be modeled. The change in potential energy calculated from the virtual crack front advance is doubled to compute the correct contour integral values.
|
||
|
||
Input File Usage: Use the following option to indicate that the crack is defined on a symmetry plane: \*CONTOUR INTEGRAL, CONTOURS=n, SYMM
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front and crack tip or crack line, and specify the crack extension direction: General: toggle on On symmetry plane (half-crack model)
|
||
|
||
# Constructing a fracture mechanics mesh for small-strain analysis with the conventional finite element method
|
||
|
||
Sharp cracks (where the crack faces lie on top of one another in the undeformed configuration) are usually modeled using small-strain assumptions. Focused meshes, as shown in Figure 11.4.2–1, should
|
||
|
||
<!-- source-page: 962 -->
|
||
|
||
normally be used for small-strain fracture mechanics evaluations. However, for a sharp crack the strain field becomes singular at the crack tip. This result is obviously an approximation to the physics; however, the large-strain zone is very localized, and most fracture mechanics problems can be solved satisfactorily using only small-strain analysis.
|
||
|
||
The crack-tip strain singularity depends on the material model used. Linear elasticity, perfect plasticity, and power-law hardening are commonly used in fracture mechanics analysis. Power-law hardening has the form
|
||
|
||
$$
|
||
\frac {\bar {\varepsilon}}{\varepsilon_ {0}} = \alpha \left(\frac {\bar {\sigma}}{\sigma_ {0}}\right) ^ {n},
|
||
$$
|
||
|
||
where is the equivalent total strain, $\varepsilon _ { 0 }$ is a reference strain, is the Mises stress, $\sigma _ { 0 }$ is the initial yield stress, n is the power-law hardening exponent (typically in the range of 3 to 8; $n > 1 0$ is very close to perfect plasticity for large ), and is a material constant (typically in the range 0.5 to 1.0).
|
||
|
||
Results for pure power-law nonlinear elastic materials in a body under traction loading are proportional to the load to some power. Therefore, the fracture parameters for one geometry under a particular load can be scaled to any other load of the same distribution but different magnitude.
|
||
|
||
If the loading is proportional (the direction of the stress increase in stress space is approximately constant) and monotonically increasing, power-law hardening deformation plasticity and incremental plasticity are essentially equivalent. However, deformation plasticity is a nonlinear elastic material for which more analytical results are available. Abaqus uses the Ramberg-Osgood form of deformation plasticity (see “Deformation plasticity,” Section 23.2.13); this model is not a pure power law model, which must be considered.
|
||
|
||
# Creating the singularity
|
||
|
||
In most cases the singularity at the crack tip should be considered in small-strain analysis (when geometric nonlinearities are ignored). Including the singularity often improves the accuracy of the J-integral, the stress intensity factors, and the stress and strain calculations because the stresses and strains in the region close to the crack tip are more accurate. If r is the distance from the crack tip, the strain singularity in small-strain analysis is
|
||
|
||
$$
|
||
\begin{array}{l} \varepsilon \propto r ^ {- 1 / 2} \quad \text { for linear elasticity, } \\ \varepsilon \propto r ^ {- 1} \quad \text { for perfect plasticity, and } \\ \varepsilon \propto r ^ {- \frac {n}{n + 1}} \quad \text { for power - law hardening. } \\ \end{array}
|
||
$$
|
||
|
||
# Modeling the crack-tip singularity in two dimensions
|
||
|
||
The square root and $1 / r$ singularity can be built into a finite element mesh using standard elements. The crack tip is modeled with a ring of collapsed quadrilateral elements, as shown in Figure 11.4.2–2.
|
||
|
||
<!-- source-page: 963 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>flowchart</summary>
|
||
|
||
```mermaid
|
||
graph TD
|
||
A["isoparametric space"] -->|h| B["1"]
|
||
A -->|g| C["-1"]
|
||
A -->|h| D["1"]
|
||
A -->|g| E["-1"]
|
||
F["physical space"] -->|r| G["a, b, c"]
|
||
F -->|r| H["1"]
|
||
F -->|r| I["1"]
|
||
F -->|r| J["1"]
|
||
```
|
||
</details>
|
||
|
||
Figure 11.4.2–2 Collapsed two-dimensional element.
|
||
|
||
To obtain a mesh singularity, generally second-order elements are used and the elements are collapsed as follows:
|
||
|
||
1. Collapse one side of an 8-node isoparametric element (CPE8R, for example) so that all three nodes— $- a , b ,$ and c—have the same geometric location (on the crack tip).
|
||
2. Move the midside nodes on the sides connected to the crack tip to the 1/4 point nearest the crack tip. You can create “quarter point” spacing with second-order isoparametric elements when you generate nodes for a region of a mesh; see “Creating quarter-point spacing” in “Node definition,” Section 2.1.1.
|
||
|
||
This procedure will create the strain singularity
|
||
|
||
$$
|
||
\varepsilon \rightarrow \frac {A}{r} + \frac {B}{r ^ {1 / 2}} \quad \mathrm{as} \quad r \rightarrow 0.
|
||
$$
|
||
|
||
The $r ^ { - } { \frac { n } { n + 1 } }$ singularity cannot be created using Abaqus elements, but the combination of the $r ^ { - 1 }$ and $r ^ { - 1 / 2 }$ terms can provide a reasonable approximation for $r ^ { - \frac { n } { n + 1 } }$ .
|
||
|
||
If 4-node isoparametric elements (for example, CPE4R) are used, one side of the element is collapsed, and the two coincident nodes are free to displace independently, $\mathrm { ~ a ~ } 1 / r$ singularity is created.
|
||
|
||
If the crack region is meshed with linear elements, the position specified for the midside nodes is ignored.
|
||
|
||
# Creating a square root singularity
|
||
|
||
If nodes $a , b ,$ and c are constrained to move together, and the strains and stresses are square root singular (suitable for linear elasticity).
|
||
|
||
<!-- source-page: 964 -->
|
||
|
||
Input File Usage: \*NFILL, SINGULAR
|
||
|
||
Constrain the collapsed nodes to move together by specifying the same node number in the list of nodes forming the element or by using a linear constraint equation or multi-point constraint to tie them together.
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front and crack tip, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, single node
|
||
|
||
Creating a 1/r singularity
|
||
|
||
If the midside nodes remain at the midside points rather than being moved to the 1/4 points and nodes a, b, and c are allowed to move independently, only the singularity in strain is created (suitable for perfect plasticity).
|
||
|
||
Input File Usage: \*NFILL
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front and crack tip, and specify the crack extension direction: Singularity: Midside node parameter: 0.5, Collapsed element side, duplicate nodes
|
||
|
||
Creating a combined square root and 1/r singularity
|
||
|
||
If the midside nodes are moved to the 1/4 points but nodes a, b, and c are allowed to move independently, the singularity created is a combination of the square root and singularities. This combination is usually best for a power-law hardening material. However, since the singularity dominates, moving the midside nodes to the 1/4 points gives only slightly better results than if the nodes are left at the midside points. Since creating a mesh with the midside nodes moved to the quarter points can be difficult, it is often best to simply use the singularity.
|
||
|
||
Input File Usage: \*NFILL, SINGULAR
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front and crack tip, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, duplicate nodes
|
||
|
||
# Modeling the crack-tip singularity in three dimensions
|
||
|
||
To create singular fields, 20-node bricks and 27-node bricks can be used with a collapsed face (see Figure 11.4.2–3).The planes of the three-dimensional elements perpendicular to the crack line should be planar for the best accuracy. If they are not planar, the element Jacobian may become negative at some integration points when the midside nodes are moved to the 1/4 points. To correct this problem, move the midside nodes slightly away from the 1/4 points toward the midpoint position (the distance moved is not critical).
|
||
|
||
See “Meshing the crack region and assigning elements,” Section 31.2.7 of the Abaqus/CAE User’s Guide, for information on creating a three-dimensional fracture mechanics mesh in Abaqus/CAE.
|
||
|
||
<!-- source-page: 965 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
C3D20(RH)
|
||
2 nodes collapsed
|
||
to the same location
|
||
3 nodes collapsed
|
||
to the same location
|
||
crack line
|
||
midplane
|
||
edge plane
|
||
midside nodes
|
||
moved to 1/4 pts.
|
||
</details>
|
||
|
||
Figure 11.4.2–3 Collapsed three-dimensional element.
|
||
|
||
# Creating a square root singularity
|
||
|
||
To obtain a square root singularity, constrain the nodes on the collapsed face of the edge planes to move together and move the nodes to the 1/4 points.
|
||
|
||
If the nodes at the midplane of a collapsed 20-node brick are constrained to move together, ; therefore, the singularity is not the same on the midplane as on an edge plane. This difference causes local oscillations in the solution about the crack tip along the crack line, although normally the oscillations are not significant.
|
||
|
||
If all midface nodes and the centroid node are included in a 27-node brick and the midside and midface nodes are moved to the 1/4 points closest to the crack line, the oscillation in the local stress and strain fields can be reduced.
|
||
|
||
Input File Usage: \*NFILL, SINGULAR
|
||
|
||
Constrain the collapsed nodes to move together by specifying the same node number in the list of nodes forming the element or by using a linear constraint equation or multi-point constraint to tie them together.
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front and crack line, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, single node
|
||
|
||
# Creating a 1/r singularity
|
||
|
||
To obtain a singularity, allow the three nodes on the collapsed face to displace independently and keep the midside nodes at the midpoints.
|
||
|
||
Input File Usage: \*NFILL
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front and crack line, and specify the crack extension direction: Singularity: Midside node parameter: 0.5, Collapsed element side, duplicate nodes
|
||
|
||
<!-- source-page: 966 -->
|
||
|
||
Creating a combined square root and 1/r singularity
|
||
|
||
To obtain a combined square root and $1 / r$ singularity, allow the nodes on the collapsed face to displace independently and move the midside nodes to the 1/4 points. As in the two-dimensional case, if it is difficult to create the mesh with the nodes moved to the 1/4 points, simply use the $1 / r$ singularity.
|
||
|
||
Input File Usage: \*NFILL, SINGULAR
|
||
|
||
Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front and crack line, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, duplicate nodes
|
||
|
||
# Mesh refinement
|
||
|
||
The size of the crack-tip elements influences the accuracy of the solutions: the smaller the radial dimension of the elements from the crack tip, the better the stress, strain, etc. results will be and, therefore, the better the contour integral calculations will be.
|
||
|
||
The angular strain dependence is not modeled with the singular elements. Reasonable results are obtained if typical elements around the crack tip subtend angles in the range of $1 0 ^ { \circ }$ (accurate) to 22.5° (moderately accurate).
|
||
|
||
Since the crack tip causes a stress concentration, the stress and strain gradients are large as the crack tip is approached. Path dependence in the evaluation of the J-integral may be an indication that the mesh is not sufficiently refined, but path independence does not prove mesh convergence. The finite element mesh must be refined in the vicinity of the crack to get accurate stresses and strains; however, accurate J-integral results can frequently be obtained even with a relatively coarse mesh.
|
||
|
||
In many cases if sufficiently fine meshes are used, accurate contour integral values can be obtained without using singular elements.
|
||
|
||
# Modeling the crack-tip region in shells
|
||
|
||
Focused meshes can be used, but not all of the three-dimensional shell elements in Abaqus/Standard can be collapsed. Elements S8R and S8RT cannot be degenerated into triangles; element types S4, S4R, S4R5, S8R5, and S9R5 can.
|
||
|
||
The quarter-point technique (moving the midside nodes to the quarter points to give a $1 / \sqrt { r }$ singularity for elastic fracture mechanics applications) can be used with S8R5 and S9R5 elements but not with S8R(T) elements. When the quarter-point technique is used with S9R5 elements, the midface node should be moved to the quarter-point position along with the two midside nodes.
|
||
|
||
If S8R(T) elements are used, a keyhole should be introduced at the crack tip.
|
||
|
||
Flaws lying in the plane through the thickness of a shell can be modeled using line spring elements; see “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1. In many cases line spring elements provide accurate J-integral and stress intensity values, but these elements are limited to modeling small strain and rotations. Limited modeling of plasticity is also allowed with line springs.
|
||
|
||
<!-- source-page: 967 -->
|
||
|
||
# Constructing a fracture mechanics mesh for finite-strain analysis with the conventional finite element method
|
||
|
||
In large-strain analysis (when geometric nonlinearities are included) singular elements should not normally be used. The mesh must be sufficiently refined to model the very high strain gradients around the crack tip if details in this region are required. Even if only the J-integral is required, the deformation around the crack tip may dominate the solution and the crack-tip region will have to be modeled with sufficient detail to avoid numerical problems.
|
||
|
||
Physically, the crack tip is not perfectly sharp. Therefore, it is normally modeled as a blunted notch with a radius $\mathrm { o f } \sim 1 0 ^ { - 3 } r _ { p }$ , where $r _ { p }$ is a characteristic dimension of the plastic zone ahead of the crack tip. The notch must be small enough that, at the loads of interest, the deformed shape of the notch no longer depends on the original geometry. Typically, the notch must blunt out to more than four times its original radius for the deformed shape to be independent of the original geometry. The size of the elements around the notch should be about 1/10 the notch-tip radius to obtain accurate results.
|
||
|
||
If a crack is modeled as sharp, the finite elements near the crack tip may not be able to approximate the high gradients, resulting in convergence problems. The stress and strain results around the crack tip will probably be inaccurate even if convergence is achieved. However, if the solution converges, the contour integral results should be reasonably accurate. The convergence difficulties will probably be greater in three dimensions than in two dimensions.
|
||
|
||
In situations involving finite rotations but small strains, such as bending of slender structures, a small “keyhole” around the crack tip should be modeled. If the hole is small, the results will not be affected significantly and problems in dealing with the singular strains at the crack tip will be avoided.
|
||
|
||
# Using constraints with the conventional finite element method
|
||
|
||
General multi-point constraints and linear constraint equations (“Kinematic constraints: overview,” Section 35.1.1) should not be used on nodes in the mesh regions where contour integrals are calculated unless the nodes involved in the constraint are located at the same point. The nodes at the crack tip of a focused mesh can be tied together using multi-point constraints without adversely affecting the contour integral calculations. Tying these nodes will change the singularity at the crack tip, but path independence of the contour integral will be maintained. In addition, path independence of the contour integrals will not be affected if two faces of a model are joined using MPC type TIE or a linear constraint equation, provided that all nodes of the two faces are coincident. Using multi-point constraints for mesh refinement or for applying symmetry/antisymmetry boundary conditions within the contour integral region will result in path dependence of the contour integrals. No warning or error messages are provided if this rule is violated.
|
||
|
||
# Procedures
|
||
|
||
You can request contour integrals in fracture mechanics problems that were modeled using the following procedures:
|
||
|
||
• static (“Static stress analysis,” Section 6.2.2) with both XFEM and the conventional finite element methods;
|
||
|
||
<!-- source-page: 968 -->
|
||
|
||
• quasi-static (“Quasi-static analysis,” Section 6.2.5) with the conventional finite element method only;
|
||
• steady-state transport (“Steady-state transport analysis,” Section 6.4.1) with the conventional finite element method only;
|
||
• coupled thermal-stress procedures (“Fully coupled thermal-stress analysis,” Section 6.5.3) with the conventional finite element method only; and
|
||
• crack propagation (“Crack propagation analysis,” Section 11.4.3) with the conventional finite element method only.
|
||
|
||
Contour integrals can be requested only in general analysis steps: they are not calculated in linear perturbation analyses (“General and linear perturbation procedures,” Section 6.1.3).
|
||
|
||
A crack analysis with pressure applied on the crack surfaces may give inaccurate contour integral values if geometric nonlinearity is included in a step.
|
||
|
||
# Loads
|
||
|
||
Contour integral calculations include the following distributed load types:
|
||
|
||
• thermal loads;
|
||
• distributed loads, including crack face pressure and traction loads on continuum elements as well as those applied using user subroutine DLOAD and UTRACLOAD;
|
||
• distributed loads, including surface traction loads and crack face edge loads on shell elements as well as those applied using user subroutine UTRACLOAD;
|
||
• uniform and nonuniform body forces; and
|
||
• centrifugal loads on continuum and shell elements.
|
||
|
||
Contributions to the contour integral due to concentrated loads in the domain are not included; instead, the mesh must be modified to include a small element and a distributed load must be applied to this element.
|
||
|
||
Contributions due to contact forces are not included.
|
||
|
||
# Material options
|
||
|
||
J-integral calculations are valid for linear elastic, nonlinear elastic, and elastic-plastic materials. Plastic behavior can be modeled as nonlinear elastic (“Deformation plasticity,” Section 23.2.13), but the results are generally best if the material is modeled by incremental plasticity and is subject to proportional, monotonic traction loading.
|
||
|
||
If unloading has taken place in the plastic zone around the crack tip, the J-integral will not be valid except in very limited cases.
|
||
|
||
The -integral is valid for problems involving creep (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4).
|
||
|
||
The stress intensity factor calculation is valid for cracks in homogeneous, linear elastic materials. It is also valid for an interfacial crack between two different isotropic linear elastic materials. It is not valid for any other types of materials, including user-defined materials.
|
||
|
||
<!-- source-page: 969 -->
|
||
|
||
The crack propagation direction is valid only for homogeneous, isotropic linear elastic materials.
|
||
|
||
The T-stress is valid only for homogeneous, isotropic linear elastic materials. Although the T-stress is calculated using the linear elastic material properties of the body with a crack, it is usually used with the J-integral calculated using the elastic-plastic material properties of the body (see “T -stress extraction,” Section 2.16.3 of the Abaqus Theory Guide).
|
||
|
||
If there is material discontinuity, the normal to the material discontinuity line must be specified for all nodes on the material discontinuity that will lie in a contour integral domain. The normal can be specified by defining user-specified normals (see “Normal definitions at nodes,” Section 2.1.4) for the elements on both sides of the discontinuity or by using nodal normal coordinates for the nodes on the discontinuity. Contour integral calculations cannot be performed for a crack with a material discontinuity line passing through its tip (except for an interfacial crack between two different materials). Therefore, you should be careful when specifying a normal that is not perpendicular to the virtual crack extension direction, , for the nodes at the crack tip.
|
||
|
||
# Elements
|
||
|
||
When used with XFEM, the contour integral can be evaluated only in first-order or second-order tetrahedron and first-order brick elements. The following paragraphs apply only to the conventional finite element method.
|
||
|
||
The contour integral evaluation capability in Abaqus/Standard assumes that the elements that lie within the domain used for the calculations are quadrilaterals in two-dimensional or shell models or bricks in continuum three-dimensional models. Triangles, tetrahedra, or wedges should not be used in the mesh that is included in the contour integral regions. When the elements around the crack tip are generated in Abaqus/CAE, triangular elements (in two dimensions) or wedge elements (in three dimensions) are converted to collapsed quadrilateral or hexahedral elements. The elements within the contour domain should be of the same type.
|
||
|
||
In shell structures the contour integrals calculated by Abaqus/Standard will be contour independent only if the deformation mode around the crack tip is primarily membrane. If there are significant bending or transverse shear effects in the domain, the contour integrals may not be contour independent and contour integral values should be obtained directly from the displacements and/or the stresses.
|
||
|
||
Generalized plane strain elements, generalized axisymmetric elements with twist, asymmetricaxisymmetric elements, membrane elements, and cylindrical elements should not be used in the contour integral regions.
|
||
|
||
The contribution of rebar is included only in the calculations of the J-integral and the -integral for shell elements defined with a shell section integrated during the analysis (see “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5).
|
||
|
||
# Output
|
||
|
||
The domain associated with each contour is calculated automatically. The nodes belonging to each domain can be printed in the data file; see “Controlling the amount of analysis input file processor information written to the data file” in “Output,” Section 4.1.1. If you are using the conventional contour integral method, for each domain Abaqus/Standard creates a new node set in the output database to include these nodes; you can view these node sets in Abaqus/CAE. In addition, new node sets are
|
||
|
||
<!-- source-page: 970 -->
|
||
|
||
created in the output database for nodes on crack surfaces and on free surfaces whose nodal normals are calculated by Abaqus/Standard.
|
||
|
||
Contour integrals cannot be recovered from the restart file as described in “Output,” Section 4.1.1.
|
||
|
||
You should not request element output extrapolated to the nodes (“Element output” in “Output to the data and results files,” Section 4.1.2) for second-order elements with one collapsed side in two dimensions or one collapsed face in three dimensions.
|
||
|
||
# Default contour integral output
|
||
|
||
By default, the contour integral values are written to the data file and to the output database file. The following naming convention is used for contour integrals written to the output database:
|
||
|
||
integral-type: abbrev-integral-type at history-output-request-name\_crack-name\_internalcrack-tip-node-set-name\_\_Contour\_contour-number
|
||
|
||
where integral-type can be
|
||
|
||
• Crack propagation direction (Cpd)
|
||
• J-integral (J)
|
||
• J-integral estimated from Ks (JKs)
|
||
• Stress intensity factor K1 (K1)
|
||
• Stress intensity factor K2 (K2)
|
||
• T-stress (T)
|
||
|
||
For example,
|
||
|
||
J-integral: J at JINT\_CRACK\_CRACKTIP-1\_\_Contour\_1
|
||
|
||
# Writing the contour integrals to the results file
|
||
|
||
You can choose to write the contour integral values to the results file in addition to the data file.
|
||
|
||
<table><tr><td>Input File Usage:</td><td>Use the following option to write the contour integrals to the results file instead of the data file:*CONTOUR INTEGRAL, CONTOURS=n, OUTPUT=FILEUse the following option to write the contour integrals to the results file in addition to the data file:*CONTOUR INTEGRAL, CONTOURS=n, OUTPUT=BOTH</td></tr><tr><td>Abaqus/CAE Usage:</td><td>You cannot write contour integrals to the results file from Abaqus/CAE.</td></tr></table>
|
||
|
||
# Controlling the output frequency
|
||
|
||
You can control the output frequency, in increments, of contour integrals. By default, the crack-tip location and associated quantities will be printed every increment. Specify an output frequency of 0 to suppress contour integral output.
|
||
|
||
The output frequency for contour integral output to the output database is controlled by the larger of the frequency values specified for history output to the output database (see “Output to the output
|